1.1 Selection of Sheet Metal Materials
Sheet metal materials are the most commonly used materials in the structural design of communication products.
Understanding the comprehensive performance of materials and the correct material selection have an important impact on product cost, product performance, product quality, and processability.
Selection principle of sheet metal materials
1) Use common metal materials to reduce material specifications and control as much as possible within the company’s material manual;
2) In the same product, reduce the variety of materials and sheet thickness specifications as much as possible;
3) Under the premise of ensuring the function of the parts, try to use cheap materials, reduce the consumption of materials, and reduce the cost of materials;
4) For the cabinet and some large plug boxes, it is necessary to fully consider reducing the weight of the whole machine;
5) In addition to the premise of ensuring the function of the parts, it must also be considered that the stamping performance of the material should meet the processing requirements to ensure the rationality and quality of the processing of the products.
Introduction of several commonly used plates
1) Cold rolled steel sheet
Cold rolled steel sheet is the abbreviation of carbon structural steel cold rolled sheet.
It is further cold-rolled from a carbon structural steel hot-rolled steel strip into a steel sheet having a thickness of less than 4 mm.
Because it is rolled at normal temperature, no iron oxide scale is produced. Therefore, the surface quality of the cold plate is good, the dimensional accuracy is high. In addition, the annealing process make it has better mechanical properties and process performance than hot rolled steel sheets.
Commonly used grades are low carbon steel 08F and 10# steel, which have good blanking and bending properties.
2) Continuous electroplated zinc cold rolled sheet steel
Continuous electroplated zinc cold-rolled steel sheet, ie “electrolytic sheet”. Refers to the process of continuously depositing zinc from an aqueous solution of zinc salt into a pre-prepared steel strip to obtain a surface galvanized layer under the action of an electric field on an electrogalvanizing line.
Because of the limitations of the process, the coating is thin.
3) Continuous hot-dip galvanized steel sheet
Continuous hot-dip galvanized steel sheet is referred to as galvanized sheet or tinplate.
The cold-rolled continuous hot-dip galvanized steel sheet and steel strip having a thickness of 0.25 to 2.5 mm are first subjected to a flame-heated preheating furnace to burn off surface residual oil.
At the same time, an iron oxide film is formed on the surface.
Then, it is heated to 710~920 °C in a reduction annealing furnace containing H2 and N2 mixed gases to reduce the iron oxide film to sponge iron.
After the surface activated and purified strip is cooled to a temperature slightly higher than the molten zinc, it enters the zinc pot at 450-460 °C.
The surface thickness of the zinc layer is controlled by an air knife.
Finally, adopt passivation treatment with chromate solution to improve white rust resistance.
Compared with the surface of the electro-galvanized sheet, the coating is thicker and is mainly used for sheet metal parts which requiring high corrosion resistance.
4) Aluminum-zinc plate
The aluminum-zinc alloy coating of aluminum-zinc plate is composed of 55% aluminum, 43.4% zinc and 1.6% silicon at 600 ° C.
Formed a dense quaternary crystal protective layer with excellent corrosion resistance, normal service life of up to 25 years, 3-6 times longer than galvanized sheet and comparable to stainless steel.
The corrosion resistance of the aluminum-zinc plate is derived from the barrier function of aluminum and the sacrificial protection of zinc.
When zinc is sacrificed for trimming, scratching, and scratching of the coating, the aluminum forms an insoluble oxide layer that acts as a barrier.
The above 2), 3), and 4) steel plates are collectively referred to as coated steel sheets and are widely used in communication equipment. After the coated steel plate is processed, it can be no longer electroplated or painted. The incision can be directly used without special treatment, and special phosphating treatment can be performed to improve the rust resistance of the incision.
From the cost analysis, the continuous electro-galvanized steel sheet is used, and the processing plant does not need to send the parts to the electroplating, which saves plating time and transportation cost. In addition, the parts are not pickled before spraying, which improves the processing efficiency.
5) Stainless steel plate
Because of its strong corrosion resistance, good electrical conductivity, high strength, etc., it is widely used.
But we should also consider its shortcomings:
- The price of the material is very expensive, which is 4 times that of ordinary galvanized sheet;
- The material strength is high, and the tool wear on the CNC punching machine is large, which is generally not suitable for CNC punching machine processing;
- The rivet nut of the stainless steel plate should be made of high-strength special stainless steel rivet nut, which is very expensive;
- If the riveting nut is not riveted, it is often necessary to spot weld again;
- The adhesion of the surface spray is not high and the quality is not suitable for control;
- The material rebounds greatly, and the bending and stamping are not easy to ensure the shape and dimensional accuracy.
Aluminum and aluminum alloy plates
The commonly used aluminum and aluminum alloy sheets are mainly composed of the following three materials:
- rust-proof aluminum 3A21
- rust-proof aluminum 5A02
- hard aluminum 2A06
Anti-rust aluminum 3A21, which is the old brand LF21, is an AL-Mn alloy. It is the most widely used rust-proof aluminum.
The strength of this alloy is not high (only higher than industrial pure aluminum) and cannot be heat treated and strengthened.
Therefore, the cold working method is often used to improve its mechanical properties, and it has high plasticity in the annealed state, and the plasticity is good in the semi-cold hardening.
It has low plasticity, good corrosion resistance and good weldability during cold work hardening.
Anti-rust aluminum 5A02 is the old brand LF2 series AL-Mg anti-rust aluminum.
Compared with 3A21, 5A02 has higher strength, especially high fatigue strength, high plasticity and corrosion resistance.
The heat treatment cannot be strengthened, and the weldability by contact welding and hydrogen atom welding is good, and there is a tendency for crystal cracks to form during argon arc welding, and the alloy tends to form crystal cracks during cold work hardening.
The alloy has good machinability in the cold hardening and semi-cold hardening state, and the machinability is poor in the annealed state, and it can be polished.
Hard aluminum 2A06 is the old LY6, which is a commonly used hard aluminum grade.
Hard aluminum and super-hard aluminum have higher strength and hardness than ordinary aluminum alloys, and can be used as some panel materials.
However, the plasticity is poor, and the bending cannot be performed, and the bending may cause cracks or cracks in the outer rounded portion.
There are new standards for the grade and status of aluminum alloy. The standard code of the grade representation method is GB/T16474-1996, the status code is GB/T16475-1996, and the comparison table with the old standard is shown in Table 1-1 below:
Table 1-1 Comparison table of new and old aluminum alloy grades
Copper and copper alloy plates
There are two main types of commonly used copper and copper alloy sheets, copper T2 and brass H62.
Copper T2 is the most commonly used pure copper. It has a purple appearance and is also called copper. It has high electrical and thermal conductivity, good corrosion resistance and formability.
But the strength and hardness are much lower than brass, and the price is very expensive.
It is mainly used as a corrosion element for conductive, heat conduction and consumer goods. It is generally used for parts on the power supply that need to carry large currents.
rass H62, which is a high-zinc brass, has high strength and excellent cold and hot workability and is easily used for various forms of press working and cutting.
Mainly used for various deep drawing and bending force parts, its conductivity is not as good as copper, but it has better strength and hardness, and the price is relatively moderate.
In the case of meeting the electrical conductivity requirements, brass H62 instead of copper is used as much as possible, which can greatly reduce the material cost.
For example, busbars, most of the current busbars are made of brass H62, which proved to be fully satisfactory.
The influence of materials on sheet metal processing
There are three main types of sheet metal processing: punching & blanking, bending, and stretching.
Different processing techniques have different requirements for the sheet.
The selection of sheet metal should also be based on the general shape and processing technology of the product.
The impact of materials on blanking
Blanking requires that the sheet should be sufficiently plastic to ensure that the sheet does not crack when punched.
Soft materials (such as pure aluminum, rust-proof aluminum, brass, copper, low-carbon steel, etc.) have good punching performance, and parts with smooth cross section and small inclination can be obtained after punching;
Hard materials (such as high carbon steel, stainless steel, hard aluminum, super-hard aluminum, etc.) have poor quality after punching, and the unevenness of the section is large, especially for thick sheets.
For brittle materials, tearing is likely to occur after punching, and particularly in the case of a small width, tearing is likely to occur.
The effect of materials on bending
Plates that need to be bent and formed should have sufficient plasticity and a low yield limit.
A highly plastic sheet that is less prone to cracking when bent.
Sheets with lower yield limit and lower modulus of elasticity have less springback deformation after bending, and it is easy to obtain an accurate curved shape.
Plastic materials such as low carbon steel, brass and aluminum with a carbon content of <0.2% are easily bent and formed;
More brittle materials, such as phosphor bronze (QSn6.5 ~ 2.5), spring steel (65Mn), hard aluminum, super-hard aluminum, etc., must have a large relative bending radius (r / t) when bending, otherwise cracking is prone to occur during bending.
Special attention should be paid to the choice of the hard and soft state of the material, which has a great influence on the bending properties.
For many brittle materials, the bending can cause the outer radius to crack or even break.
There are also some steel plates with higher carbon content. If you choose a hard state, the bending will also cause cracking or even fracture of the outer radius. These should be avoided as much as possible.
Effect of materials on drawing processing
The stretching of the sheet, especially the deep drawing, is a difficult one in the sheet metal processing process.
Not only the depth of the stretching is required to be as small as possible, the shape is as simple as possible and smooth. Besides the material is required to have good plasticity. Otherwise, the whole part is easily deformed, partially wrinkled, or even pulled at the stretching portion.
The yield limit is low and the directional coefficient of the plate thickness is large. The smaller the yield ratio σs/σb of the sheet, the better the punching performance and the greater the limit of the primary deformation.
When the plate thickness directivity coefficient >1, the deformation in the width direction is easier than the deformation in the thickness direction.
The larger the value of stretch radius R, the less likely it is to be thinned and fractured during the stretching process, and the better the tensile properties.
Common tensile properties are: pure aluminum sheet, 08Al, ST16, SPCD.
Material impact on stiffness
In the design of sheet metal structure, the rigidity of sheet metal structural parts is often not met.
Structural designers often use low carbon steel or stainless steel instead of low carbon steel, or replace the ordinary aluminum alloy with a hard aluminum alloy with high strength and hardness, and it is expected to increase the rigidity of the part.
There is actually no obvious effect.
For materials of the same substrate, the strength and hardness of the material can be greatly improved by heat treatment and alloying.
But the change in stiffness is small.
To improve the rigidity of the part, only by changing the material and the shape of the part can a certain effect be achieved.
See Table 1-2 for the elastic modulus and shear modulus of different materials.
Table 1-2 Elastic Modulus and Shear Modulus of Common Materials
|Elastic Modulus E||Shear Modulus G|
|Grey cast iron||118~126||44.3|
|Carbon steel, Nickel-chromium steel||206||79.4|
|Rolled pure copper||108||39.2|
|Cold drawn pure copper||127||48|
|Rolled phosphor bronze||113||41.2|
|Cold drawn brass||89~97||34.3~36.3|
|Rolled manganese bronze||108||39.2|
|Pull out aluminum wire||69|
|Cast aluminum bronze||103||11.1|
|Cast tin bronze||103|
|Hard aluminum alloy||70||26.5|
|Low pressure polyethylene||0.54~0.75|
|High pressure polyethylene||0.147~0.24|
Performance comparison of commonly used plates
Table 1-3 Comparison of performance of several commonly used plates
|Price coefficient||Lap resistance (mΩ)||CNC punching processing performance||Laser processing performance||Bending performance||Rivet nut technology||Pressing rivet technology||Surface coating||Incision protective performance|
|3||46||Average||extreme poor||extreme poor||good||good||Average||good|
- The data in the table is related to the specific grade of the material and the manufacturer, and is only used as a qualitative reference.
- Aluminum alloy and copper alloy sheets are extremely poor in laser cutting, and laser processing is generally not available.
1.2 Piercing and Blanking
Common way of piercing and blanking
Piercing and blanking by CNC punch press
CNC punching and blanking is to use the single-chip microcomputer on the CNC punching machine to input the machining program (size, machining path, processing tool, etc.) of the sheet metal part in advance, which makes the CNC punching machine adopts various tools and a wealth of NC commands to achieve a variety of forms of processing like punching, trimming, forming etc.
CNC punching generally cannot achieve piercing and blanking with too complicated shapes.
- High speed
- Flexible processing
It basically able to meet the needs of sample blanking production.
Attention problems and requirements:
- Thin material (t<0.6) is not easy to process, and the material is easy to deform;
- The processing range is limited by tools, jaws, etc.
- Moderate hardness and toughness have better piercing performance;
- Too high hardness will increase the piercing force and have a bad influence on the punchhead and precision;
- The hardness is too low, which causes severe deformation during piercing and the accuracy is greatly limited;
- High plasticity is advantageous for forming, but it is not suitable for encroaching, continuous punching, and it is not suitable for punching and trimming;
- Appropriate toughness is beneficial for punching, which suppresses the degree of deformation during punching;
- If the toughness is too high, the rebound will be severe after punching, which will affect the accuracy.
CNC punching is generally suitable for punching low carbon steel, electrolytic plate, aluminum-zinc plate, aluminum plate, copper plate with T=3.5~4mm or less, and stainless steel plate with T=3mm or less.
The recommended sheet thickness for CNC punching is:
- The aluminum alloy plate and the copper plate are 0.8～0mm
- The low carbon steel plate is 0.8～5 mm
- Stainless steel plate 0.8~2.5mm
The CNC punching process has a large deformation on the copper plate, while the processing PC and the PVC plate have large processing edge burrs and low precision.
When punching, the diameter and width of the tool used must be greater than the thickness of the material. For example, a tool with a diameter of Φ1.5 cannot punch a material of 1.6 mm.
Materials below 0.6mm are generally not processed by NCT.
Stainless steel materials are generally not processed by NCT. (Of course, 0.6~1.5mm material can be processed by NCT, but the tool wear is large, and the probability of scrap rate in the field processing is much higher than other GI materials.)
Piercing and blanking of other shapes are desirably as simple and uniform as possible.
The size of the CNC punch should be normalized, such as round holes, hexagonal holes, and the minimum width of the process groove is 1.2mm.
Piercing and blanking by cold punch die
For punching and blanking of parts with large output and small size, specially designed sheet metal stamping dies are made and used for increased production efficiency.
It generally consists of a punch and a die.
The die is generally include: press-in type, inlaid type.
Punches are generally include: round type, can be replaced; combined type; quick loading and unloading type.
The most common dies are:
- Blanking die (mainly: open blanking die, closed blanking die, piercing& blanking compound die, open punching blanking continuous die, closed punching blanking continuous die)
- Bending die
Because the punching and blanking with cold die can basically be completed by one stamping, the efficiency is high, the consistency is good, and the cost is low.
Therefore, for the structural parts with an annual processing capacity of more than 5,000 pieces and the part size is not too large, the processing plant generally performs cold die processing.
In the design of the structure, it is necessary to consider the design of the process characteristics of the cold die processing.
For example, the parts should not have sharp corners (except for use). They should be designed to be rounded to improve the quality and life of the mold, and make the workpiece beautiful, safe and durable.
In order to meet the functional requirements, the structural shape of the part can be designed to be more complicated.
Piercing by dense hole punch
The dense hole punch can be regarded as a kind of numerical control punch. For parts with a large number of dense holes, the punching efficiency and precision can be improved.
Specially made punching die can punch a large number of dense holes to process the workpiece.
Such as: ventilation stencil, inlet and outlet air baffle.
See Figure 1-1.
Figure 1-1 Schematic diagram of dense hole punching
The shaded part in the figure is a dense hole mold, and the dense hole of the part can be quickly punched out by the dense hole mold. Compared to one punch, it greatly improves efficiency.
Problems and requirements for dense holes arrangement designs
The design of the dense hole on the product should consider that the processing characteristics of the dense hole punching die is repeated multiple times of punching, so the following principle should be adopted when designing the arrangement of the dense hole:
- When designing the dense hole arrangement, first consider the planned dense hole die to reduce the mold cost;
- The same type of dense hole arrangement should be uniform, the line spacing should be defined by a constant value, and the column spacing also defines a constant value, so that the same type of dense hole mold can be used universally, reducing the number of mold opening and reducing the mold. the cost of;
- The size of the same type of hole should be the same. For example, the hexagonal hole can be unified into the hexagonal hole with the inscribed circle Φ5. This hexagonal hole is the common size of the company’s hexagonal hole, accounting for more than 90% of the hexagonal hole.
- When the number of holes in the two rows is not equal, two requirements must be met: 1. The hole pitch is larger, the edge distance of the two holes is greater than 2t (t is the material thickness); 2. The total number of rows should be evenly arranged. , as shown in Figure 1-2;
Figure 1-2 Schematic diagram of misalignment of dense holes
- If the hole pitch of the dense hole is small, the number of holes in each row must be an even number. As shown in Figure 1-3, when the distance D between two dense holes is less than 2t (t is the material thickness), the dense hole molds should be spaced apart due to the strength of the mold. The shaded part in the figure is a dense hole mold. It can be seen that the number of holes per row must be an even number. If the hole pitch in Figure 1-2 is also very small, because the number of holes in each row is not equal (7 empty, 8 holes), it cannot be punched out once with a dense hole die.
Figure 1-3 dense hole mold
The dense hole mold of Figure 1-1 a can be designed as shown in Figure 1-4.
Figure 1-4 dense hole mold
The dense hole mold of Figure 1-1 b can only be designed as shown in Figure 1-5.
Figure 1-5 dense hole mold
When designing the arrangement of dense holes, try to design according to the above requirements, and continuous and have certain regularity, which is convenient for opening the hole mold and reducing the stamping cost. Otherwise, only a few punches or a number of sets of molds can be used to complete the processing.
As shown in Figure 1-6,
- Figure a, staggered holes, the number of rows is not even;
- Figure b, the holeis missing in the middle;
- Figure c, the dense hole distance is too close, the number of holes per row and the number of holes per column are odd;
- Figure d&e, the dense hole distance is too close, the number of holes in each rowof the dense hole is not equal, these can not be completed only by the punching of the dense hole die, and must be completed by other complementary processing methods.
- Figure f,If it is machined with a dense hole mold, it needs to be completed by other supplementary processing methods. Even if the material blanking mold is made, multiple hole punching molds are required to complete, and the processability is poor.
Figure 1-6 Schematic diagram of the dense hole arrangement
Laser cutting is a non-contact cutting technology that uses electron discharge as a source of energy to focus a laser beam as a heat source by using a reflecting mirror group. This high-density light energy is used to achieve punching and blanking of sheet metal parts.
- Diversified cutting shapes
- Cutting speed is faster than wire cutting
- Small heat affected zone
- Material will not be deformed
- Small incision
- High precision and quality
- Small noise
- No tool wear
- No need to consider the hardness of the cutting material
- It can process large, complex shapes and parts that are difficult to machine by other methods.
However, the cost is high, and the support table of the workpiece is damaged at the same time, and the cut surface is easy to deposit an oxide film, which is difficult to handle. Generally only suitable for single and small batch processing.
Attention : generally only used for steel plates.
Aluminum plates and copper plates are generally not used because the material heat transfer is too fast, causing melting around the incision, which does not guarantee processing accuracy and quality.
The laser cutting end face has a layer of oxide scale, which can not be washed off, and the cutting end face with special requirements should be polished;
Laser cutting dense holes are more deformed, generally do not use laser to cut dense holes.
Wire cutting is a processing method in which a workpiece and a wire (molybdenum wire, copper wire) are each used as a pole and kept at a certain distance, and a spark gap is formed when a voltage is high enough, and the workpiece is subjected to electrolytic etching. The removed material is carried away by the working fluid.
Features: high processing accuracy, but low processing speed, high cost, and will change the surface properties of the material.
Generally used for mold processing, not used for processing production parts.
Some square holes of the profile panels have no rounded corners that cannot be milled, and because aluminum alloys cannot be cut by laser, if there is no punching space, they can only be punched by wire EDM.
The speed is very slow, the efficiency is very low, and it is not suitable for mass production. The design should avoid this situation.
Comparison of the three commonly used blanking and piercing methods
Table 1-4 Comparison of three common punching and blanking processing characteristics
Note: The following data is data for cold rolled steel sheets.
|Machinable material||steel plate||Steel plate, copper plate, aluminum plate||Steel plate, copper plate, aluminum plate|
|Machinable material thickness||1mm ～ 8mm||0.6mm ～ 3mm||generally ＜4mm|
|Processing minimum size (normal cold rolled steel plate)||Minimum slit 0.2mm||Punching hole Ø≧t||Punching hole Ø≧t|
|Minimum circle 0.7mm||Square hole small edge W≧t||Square hole small edge W≧t|
|Long groove width W≧t||Long groove width W≧2t|
|Minimum distance between hole and hole, hole and edge||≧t||≧t||≧1t|
|Preferably the distance between the holes and holes,holes and the edges||≧1.5t||≧1.5t||≧1.5t|
|General machining accuracy||±0.1mm||±0.1mm||±0.1mm|
|Appearance effect||Smooth outer edge, a layer of scale on the cut end face||Large raw edges with burrs||a small amount of raw edges|
|Curve effect||Smooth, changeable shape||Large burrs and regular shapes;||Smooth, changeable shape|
|Processing speed||Cutting the outer circle quickly||Punching dense holes fast||fastest|
|Processing text||Etching, shallower, unlimited size||Stamped concave text with deeper symbols; size is limited by the mold||Stamped concave text with deeper symbols; size is limited by the mold|
|Forming||can’t||Concave, counterbore, small stretch, etc.||Can achieve more complex shapes|
Process design of piercing and blanking
Technical design of arrangement
In large-volume and medium-volume production, the material cost of parts accounts for a large proportion.
The full and effective use of materials is an important economic indicator for sheet metal production.
Therefore, under the condition that the design requirements are not affected, the structural designer should strive to adopt the arrangement method without waste or less waste.
As shown in Figure 1-7, there is no waste arrangement.
Figure 1-7 No waste arrangement
Some parts have a slightly changed shape, which can save a lot of material.
As shown in Figure 1-8, Figure 2 uses less material than Figure 1.
Figure 1-8 A slightly modified design of the material arrangement
Processability of blanking parts
For the CNC punching machine to process the outer radius, a special external tool is required. In order to reduce the outer circle tool, the standard corner rounding of this manual as shown in Figure 1-9 is:
1) 90 degree right angle corner rounding series, the radius is r2.0, r3.0, r5.0, r10
2) The 135 degree beveled corner radius is uniform to R5.0
Figure 1-9 The outer corner rounding of the blank
Punching is preferred to use round holes. The round holes should be selected according to the series of round holes specified in the sheet metal mold manual. This can reduce the number of round hole tools and reduce the time for blade changing on CNC punching.
Due to the punch strength limitations, the aperture cannot be too small. Its minimum aperture is related to the material thickness.
The minimum diameter of the hole should not be less than the value shown in Table 1-5 below.
Table 1-5 Minimum size for punching with a common punch
|The minimum diameter or minimum edge length of the punch (t is the material thickness)|
|Material||Round hole D（D is diameter）||Square hole L（L is edge length）||Waist hole, rectangular hole a（a is hte min edge length）|
|High and medium carbon steel||≥1.3t||≥1.2t||≥1t|
|Low carbon steel and brass||≥1t||≥0.8t||≥0.8t|
|Cloth bakelite laminate||≥0.4t||≥0.35t||≥0.3t|
The distance between the holes, and between the hole and the edge should not be too small. The value is shown in Figure 1-10:
Figure 1-10 The distance between the holes, the hole and the edge of the blanking parts
The precision between the hole and the shape, the hole and the hole processed by the composite mold is easy to ensure during the stamping process of the mold. Besides, the processing efficiency is high, and the maintenance cost of the mold is convenient for maintenance.
Considering the above reasons, the distance between the hole and the hole, if the distance between the hole and the shape can meet the minimum wall thickness requirement of the composite mold, the process is better, as shown in Figure 1-11:
Figure 1-11 Edge requirements for blanking parts
Table 1-6 Minimum size of the edge of the composite die blanking
|t (＜0.8 )||t (0.8~1.59)||t (1.59~3.18)||t (＞3.2)|
As shown in Figure 1-12, first piercing and then bending. In order to ensure that the hole is not deformed, the minimum distance between the hole and the flange X≥2t+R
Figure 1-12 Minimum distance between a hole and a flange
When punching holes on the deep drawing parts, see Figure 1-13, in order to ensure the shape and positional accuracy of the holes and the strength of the mold, the hole wall and the straight wall of the parts should be kept at a certain distance, that is, the distances a1 and a2 should meet the following requirements:
- a1 ≥R1+0.5t
In the formula, R1, R2 is the corner radius, and t is the thickness.
Figure 1-13 Punching on the deep drawing parts
Processing precision of blanking parts
Figure 1-14 Tolerance of the center distance of the hole of the blanking parts
Table 1-7 Tolerance Table of Hole Center Distance (Unit:mm)
|Ordinary punching accuracy||Advanced punching accuracy|
|Nominal size L||Nominal size L|
Note: All holes should be punched out once when using the values in this table.
Figure 1-15 Tolerance of hole center to edge distance
Selection principle of stamping part design size
1) The design dimensional reference of the stamped part is as close as possible to the manufactured positioning reference, so that the manufacturing error of the dimension can be avoided.
2) The hole size reference of the stamping part should be selected as far as possible from the beginning to the end of the stamping process, and should not be associated with the part participating in the deformation.
3) For parts that are dispersed and stamped on different molds in multiple steps, the same positioning reference should be used as much as possible.
Table 1-8 Tolerance table of hole center and edge distance
Note: This table is suitable for hole punching after blanking.
Secondary cutting is also called secondary blanking, or additional cutting (very poor process, should be avoided when designing).
The secondary cutting is that the stretching has a deformation of the material. When the bending deformation is large, the blanking is increased. Forming first, then cutting holes or contours to remove the reserved material and obtain the complete correct structure size.
Application: when the tensioning boss is close to the edge, additional cut must be performed.
Take the counterbore as an example, as shown in Figure 1-16.
Figure 1-16 Secondary cutting
1.3 Bending of Sheet Metal Parts
Sheet metal bending refers to the processing of changing the angle of a sheet or panel.
For example, the plate is bent into a V shape, and U shape.
In general, there are two ways to bend a sheet metal:
One method is mold bending, which is used for sheet metal parts with complicated structure, small volume and large batch processing;
The other is press brake bending which is applied to the sheet metal structure with a relatively large structural size or a small yield.
These two bending methods have their own principles, characteristics and applicability.
Bending by mold
For structural parts with an annual processing capacity of more than 5,000 pieces and a part size not too large (generally 300X300), the processing manufacturer generally considers the mold bending.
Common bending mold
Commonly used bending dies, as shown in Figure 1-17: In order to extend the life of the mold, the parts should be designed with rounded corners.
Figure 1-17 Special Forming Mold
Too small a flange height, that is, the use of a bending die is also not conducive to forming, generally the height of the flange is L ≥ 3t (including the wall thickness).
Step processing method
Some of the lower-profile sheet metal Z-shaped steps are bent, and the processing manufacturers often use simple molds to machine on punch presses or hydraulic presses.
If the batch size is not large, it can be processed by the step die on the bending machine, as shown in Figure 1-18.
However, its height H cannot be too high and should generally be between (0～1.0) t.
If the height is (1.0～4.0) t, it is necessary to consider the mold form of the unloading structure according to the actual situation.
This mold step height can be adjusted by adding a spacer.
Therefore, the height H is arbitrarily adjusted.
However, there is also a disadvantage in that the length L size is not easily ensured, and the verticality of the vertical side is not easily ensured.
If the height H is large, consider bending on the press brake machine.
Figure 1-18 Z-shaped step bending
Bending by press brake machine
The bending machine is divided into two types: ordinary bending machine and CNC bending machine.
Due to the high precision requirements and the irregular shape of the bend, the sheet metal bending of the communication device is generally bent by a numerical control bending machine.
The basic principle is to bend and shape the sheet metal part by using the bending punch (upper mold) and the V-shaped die (lower mold) of the bending machine.
Convenient clamping, accurate positioning and fast processing speed;
The bending force is small, and it can only be processed by simple forming, and the efficiency is low.
Basic principles of forming
The basic principle of forming is shown in Figure 1-19:
Figure 1-19 Basic principle of forming
1) Bending knife (upper die)
The form of the bending knives is shown in Figure 1-20. The machining is mainly based on the shape of the workpiece.
Generally, the processing tool has a large number of bending knives. In particular, the manufacturers with a high degree of specialization will custom-made bending knives of many shapes and specifications in order to process a variety of complex bending, .
2) Lower die
The lower mold is generally V=6t (t is the material thickness).
There are many factors affecting the bending process, including the arc radius of the upper die, the material, the thickness of the material, the strength of the lower die, and the vee opening size of the lower die.
In order to meet the demand of the products, the manufacturer has already serialized the bending die in the case of ensuring the safety of the bending machine.
You need to have a general understanding of the existing bending die during the structural design process.
See Figure 1-20. The left side is the upper mold and the right side is the lower mold.
Figure 1-20 Schematic diagram of the press brake punch and die
The basic principle of the bending process sequence:
1) Bending from the inside to the outside;
2) Bending from small to large;
3) Bend the special shape first and then bend the general shape;
4) After the previous process is formed, it does not affect or interfere with the subsequent process.
The bending forms seen by the current outsourcing factory are generally shown in Figure 1-21.
Figure 1-21 Bending form of press brake machine
When the sheet metal is bent, a bend radius is required at the bend.
The bending radius should not be too large or too small and should be chosen appropriately.
If the bending radius is too small, the bending will be cracked, and if the bending radius is too large, the bending is easy to rebound.
The preferred bending radius (inside bending radius) of various materials with different thicknesses is shown in Table 1-9 below.
|Material||Annealed state||Cold work hardening state|
|Corresponding position of the direction of the bending line and the direction of the fiber|
|08,10||0.1t||0.4 t||0.4 t||0.8 t|
|15,20||0.1 t||0.5 t||0.5 t||1.0 t|
|25,30||0.2 t||0.6 t||0.6 t||1.2 t|
|45,50||0.5 t||1.0 t||1.0 t||1.7 t|
|65Mn||1.0 t||2.0 t||2.0 t||3.0 t|
|Aluminum||0.1 t||0.35 t||0.5 t||1.0 t|
|Copper||0.1 t||0.35 t||1.0 t||2.0 t|
|Soft brass||0.1 t||0.35 t||0.35 t||0.8 t|
|Semi-hard brass||0.1 t||0.35 t||0.5 t||1.2 t|
|Phosphor bronze||——||——||1.0 t||3.0 t|
Note: t is the thickness of the sheet in the table.
The data in the above table is the preferred data and is for reference only.
In fact, the manufacturer’s bending knives usually have a rounded corner of 0.3, and a small number of bending knives have a rounded corner of 0.5.
Therefore, the bending inner radius of our sheet metal parts is basically 0.2.
For ordinary low carbon steel plates, rust-proof aluminum plates, brass plates, copper plates, etc., the inner radius 0.2 is no problem.
However, for some high carbon steel, hard aluminum, super hard aluminum, this rounded corner will cause the bend to break or the outer corner to crack.
Figure 1-22 Bending and rebounding diagram
1) Rebound angle Δα=b-a
In the formula formula:
- b-the actual angle of the workpiece after rebound;
- a-the angle of the mold.
2) The size of the rebound angle
The rebound angle at 90° free bend is shown in Table 1-10.
Table 1-10 Rebound angle at 90 degree free bend
|Medium carbon steel σb=400-500MPa||<1||5°||2°||0°|
|Hard yellow copper σb=350-400MPa||1~5||6°||3°||1°|
|Hard bronze σb=350-400MPa||>5||8°||5°||3°|
|High carbon steel σb>550Mpa||<1||7°||4°||2°|
- Factors affecting rebound and measures to reduce rebound.
- Mechanical properties of the material
The size of the rebound angle is proportional to the yield point of the material and inversely proportional to the elastic modulus E.
For sheet metal parts with high precision requirements, in order to reduce the rebound, the material should be as low-carbon steel as possible, not high carbon steel and stainless steel.
- The larger the relative bending radius r/t, the smaller the degree of deformation, and the larger the rebound angle Δα.
This is a more important concept.
The rounded corners of sheet metal bends should be selected with a small bend radius as much as possible, which is beneficial to improve the accuracy.
In particular, it should be avoided to design large arcs as much as possible, as shown in Figure 1-23. Such large arcs are more difficult for production and quality control.
Figure 1-23 The arc of the sheet metal is too large
Calculation of the minimum bend edge of a bend
The initial state of the bend of the L-shaped bend is shown in Figure 1-24:
Figure 1-24 L-bend bending
One important parameter here is the width B of the lower die.
Due to the bending effect and the strength of the mold, there is a minimum of the width of the die required for materials of different thicknesses.
When it is less than this value, there will be a problem that the bending is not in place or the mold is damaged.
It has been proved by practice that the relationship between the minimum die width and the material thickness is:
Bmin = kT ①
Bmin is the minimum mold width, T is the material thickness, and K=6 when calculating the minimum die width.
At present, the specifications of the bending die width commonly used by manufacturers are as follows:
4, 5, 6, 8, 10, 12, 14, 16, 18, 20, 25
According to the above relationship, the minimum thickness of the lower die width required for different material thicknesses during bending can be determined.
For example, when a 1.5mm thick plate is bent, B=6*1.5=9. For the die width series above, you can choose a die width of 10mm (or 8mm) of the lower die.
From the initial state diagram of the bend, it can be seen that the edge of the bend cannot be too short. Combined with the minimum die width above, the formula for obtaining the shortest bend edge is ②: (see Figure 1-25)
Lmin is the shortest bent edge, Bmin is the minimum die width, and Δ is the bending coefficient of the sheet.
When the 1.5mm thick plate is bent, the shortest bend edge Lmin = (8 + 2.5) / 2+0.5 = 5.75mm (including a plate thickness).
Figure 1-25 Minimum die width
Table 1-11: Inner bending radius of cold rolled steel sheet material R and minimum bending height reference table
|No.||Thickness||V opening||Punch radius R||Min bending height|
|3||0.8||5||0.8 or 0.2||3.7|
|4||1||6||1 or 0.2||4.4|
|5||1.2||8（or 6）||1 or 0.2||5.5（or 4.5）|
|6||1.5||10（or 8）||1 or 0.2||6.8（or 5.8）|
|7||2||12||1.5 or 0.5||8.3|
|8||2.5||16（or 14）||1.5 or 0.5||10.7（or 9.7）|
|9||3||18||2 or 0.5||12.1|
- The minimum bend height contains a material thickness.
- When the V-bend is an acute angle, the shortest bend must be increased by 0.5.
- When the part material is aluminum plate and stainless steel plate, the minimum bending height will have a small changes. The aluminum plate will become smaller, the stainless steel will be larger, refer to the above table….
Minimum bend height for Z-bends
The initial state of the Z-bend bend is shown in Figure 1-26:
The Z-bend and L-bend processes are very similar, and there is also a minimum bend edge problem. Due to the structure of the lower die, the shortest edge of the Z-bend is larger than the L-bend.
The formula for calculating the minimum edge of a Z-bend is:
Lmin=1/2(Bmin+Δ)+D + 0.5 + T ③
Lmin is the shortest bend edge, Bmin is the minimum mold width, Δ is the bending coefficient of the sheet, T is the material thickness, and D is the structural size of the lower die to the edge, generally greater than 5mm.
Figure 1-26 Z-bend
The minimum bend size L for sheet metal Z-bends of different material thicknesses is shown in Table 1-12 below:
Table 1-12 Minimum height of Z bend
|No||Thickness||V opening||Punch radius R||Z -bend height L|
|3||0.8||5||0.8 or 0.2||9.5|
|4||1||6||1 or 0.2||10.4|
|5||1.2||8（or 6）||1 or 0.2||11.7（or 10.7）|
|6||1.5||10（or 8）||1 or 0.2||13.3（or 12.3）|
|7||2||12||1.5 or 0.5||14.3|
|8||2.5||16（or 14）||1.5 or 0.5||18.2（or 17.2）|
|9||3||18||2 or 0.5||20.1|
Interference during bending
For secondary or above secondary bending, it is often the case that the bending workpiece interferes with the tool.
As shown in Figure 1-27, the black part is the interference part, so that the bending cannot be completed, or the bending deformation is caused by the bending interference.
Figure 1-27 Interference of bending
The interference problem of sheet metal bending does not involve too much technology.
Just understand the shape and size of the bending die, and avoid the bending die when designing the structure.
Figure 1-28 shows the cross-sectional shapes of several common bending knives, which are described in the sheet metal mold manual, and there are corresponding tool entities in the intralink library.
In the case of unsure design, the assembly interference test can be directly performed with the tool according to the principle of the above figure.
Figure 1-28 Bending knife
For flip hole tapping, the D value shown in Figure 1-29 cannot be designed too small.
The minimum D value can be calculated or plotted based on material thickness, through hole outer diameter, flange hole height, selected bending tool parameters.
For example, a flip hole tapping of a M4 with a 1.5 mm sheet bent, the D value should be greater than 8 mm. Otherwise, the bending knife will hit the flange.
Figure 1-29 Bending of the hole flanging & tapping
Minimum distance between the hole and the oblong hole
As shown in Figure 1-30, the edge of the hole at the bend is too close to the fold line. When the bend is performed, it cannot be taken up, resulting in a change in the shape of the hole.
Therefore, the hole edge and the bend line are required to be larger than the minimum hole margin X ≥ t + R.
Figure 1-30 Minimum distance from the round hole to the bend edge
Table 1-13 Minimum distance from the round hole to the bend edge
|Min Distance X||1.3||1.5||1.7||2||3||3.5|
As shown in Figure 1-31, the oblong hole is too close to the fold line. When the bend is performed, the material cannot be taken up, and the shape of the hole is deformed. Therefore, the hole edge and the bend line are required to be larger than the minimum hole margin (refer to table 1-14), the bend radius refer to Table 1-9.
Figure 1-31 The minimum distance from the long round hole to the bend edge
Table 1-14 Minimum distance from the long round hole to the bend edge
|Min distance X||2t+R||2.5t+R||3t+R|
For unimportant holes, expand the hole to the bend line, as shown in Figure 1-32.
Disadvantages: affect the appearance.
Figure 1-32 Improved bending design
Special processing when the hole is close to the bend
When the distance from the hole which close to the bend line to the bend edge is less than the minimum distance described above, deformation will occur after the bend.
At this time, according to the different requirements of the product, it can be handled as shown in the following Table 1-15.
However, it can be seen that the technicality of these methods is poor, and the structural design should be avoided as much as possible.
Table 1-15 Special processing when the hole is close to the bend
1) Pressing the groove before bending. In the actual design, because the structural design needs, the actual distance is smaller than the above distance. The processing manufacturer often performs the groove pressing before the bending, as shown in Figure 1-31. The disadvantage is: one extra process is need for the bending processing, the efficiency is lower, the precision is lower, and in principle, it should be avoided as much as possible.
2) Cut hole or line along the bend line:When the bend line has no effect on the appearance of the workpiece or is acceptable, then use hole cutting to improve its techniques.Disadvantages: affect the appearance. And when cutting a line or cutting a narrow groove, it is generally necessary to cut with a laser machine.
3) Completion to the design size after bending at the edge of the hole near the bend line. When the hole margin is required, it can be handled in this way.Generally, this secondary material removal cannot be completed on a punching machine, and the secondary cutting can only be performed on the laser cutting machine, and the positioning is troublesome, and the processing cost is high.
4) After the bending, the hole reaming process only has one or several pixel holes to the bending line and the distance is less than the minimum hole distance. When the appearance of the product is strict, in order to avoid the drawing during bending, the pixel can be performed at this time.Shrinkage treatment, that is, cutting a small concentric circle (usually Φ1.0) before bending, and reaming to the original size after bending.Disadvantages: many projects, low efficiency.
5) The minimum width of the upper die of the bending machine is 4.0mm (current). Due to this limitation, the hole in the bending part of the workpiece shall not be less than 4.0mm. Otherwise, the opening must be enlarged or use easy to form die to perform the bending.Disadvantages: low efficiency in making easy mold, low efficiency in easy mold production; reaming affects appearance.
Process holes, process slots and process notches for curved parts
When designing the bending part, if the bending part has to bend the bending edge to the inner side of the blank, the punching process hole, process groove or process notch should generally be added before blanking, as shown in Figure 1-33.
Figure 1-33 Adding punch hole, process process or process notch
D- diameter of the process hole, d ≥ t;
K-process notch width, K ≥ t.
Crack avoid groove or cut slit:
In general, for a part of an edge to bend, in order to avoid tearing and distortion, the crack avoid groove or cut slit should be opened.
Especially for bending with an inner corner of less than 60 degrees, it is necessary to open the crack groove or the slit.
The width of the slit is generally greater than the thickness t, and the depth of the slit is generally greater than 1.5t.
In the figure 1-34, Figure b is more reasonable than Figure a.
Figure 1-34 Bending of the sheet with crack groove or slit
The process groove and process hole should be processed correctly, and if the workpieces that can be seen from the panel and the appearance, then the cornering process holes of the bending can be not added (for example, the process notch is not added in the process of planel processing in order to maintain a uniform style), and other bends should add the cornering process hole, as shown in Figure 1-35.
Figure 1-35 Bending corner process hole
When designing the drawings, if there is no special requirement, do not mark the gap between the bending collisions in the 90 ° direction.
Some unreasonable gap markings affect the process design of the manufacturer.
The processing manufacturer generally designs the process according to the gap of 0.2 to 0.3. As shown in Figure 1-36:
Figure 1-36 the gap between the bend lapping
Bending of a sudden change position
The bending zone of the bending part should avoid the location of the sudden change of the part. The distance L of the bending line from the deformation zone should be greater than the bending radius r, ie L≥r, as shown in Figure 1-37
Figure 1-37 The bend zone should avoid the location of the sudden change of the part
One time hemming
The way for hemming: As shown in Figure 1-38, first fold the sheet to 30 degrees with a 30 degree bending knife, and then flatten the bent side.
Figure 1-38 Method of hemming
The minimum bend edge dimension L in the figure is 0.5t (t is the material thickness) according to the minimum bend edge size of the one bend edge described in above.
The pressed dead edge is generally applied to stainless steel, galvanized sheet, and aluminum-zinc plate.
Plating parts should not be used, because there is a phenomenon of acid trapping in the place where the hemming is performed.
180 degree bend method:
As shown in Figure 1-39, first fold the plate to 30 degrees with a 30 degree bending knife, then flatten the bending edge, and then pull out the pad.
Figure 1-39 180 degree bend method
The minimum bend edge dimension L in the figure is the minimum bend edge dimension of one bend edge plus t (t is the material thickness), and the height H should be selected from commonly used plates, such as 0.5, 0.8, 1.0, 1.2, 1.5, 2.0. Generally, this height is not suitable for selecting a higher size.
Triple folding hemming
As shown in Figure 1-40, fold the shape first, then fold the edge. Pay attention to the dimensions of each part during design to ensure that each processing step meets the minimum bending size and avoid unnecessary post-processing.
Figure 1-40 Triple folding hemming
Table 1-16 Minimum bearing edge size required for final bending edge flattening
|Bearing edge size L||4.0||4.0||4.0||4.0||4.5||4.5||5.0||5.0|
1.4 Structural Form of Nuts and Screws on Sheet Metal Parts
Common forms of riveted nuts are self-clinching standoff, self-clinching nut, anchor rivet nut, pull rivet nut, floating rivet nut.
Pressing riveting means that in the riveting process, under the external pressure, the riveting part plastically deforms the base material, and is squeezed into the prefabricated groove specially designed in the riveted screw and nut structure, thereby realizing the reliable connection of the two parts.
There are two types of non-standard nuts for riveting, one is a Self-clinching standoff and the other is a self-clinching nut.
The connection to the substrate is achieved using such a riveted form.
Such riveting forms typically require the riveted part to have a hardness greater than the hardness of the substrate.
Ordinary low carbon steel, aluminum alloy plate and copper plate are suitable for crimping the self-clinching standoff.
For stainless steel and high carbon steel sheets, because of the hard material, a special high-strength rivet nut column is required, which is not only expensive, but also difficult to crimp, and the crimping is not reliable, and it is easy to fall off after crimping.
In order to ensure reliability, manufacturers often need to add welding on the side of the nut column, which is not good in process.
Therefore, the sheet metal parts with the rivet nut column and the rivet nut are not as stainless steel as possible.
This is also the case with rivet screws and rivet nuts, which are not suitable for use on stainless steel sheets.
The crimping process of the rivet nut column is shown in Figure 1-41:
Figure 1-41 Schematic diagram of the riveting process
Self-clinching rivet nut
The crimping process of the rivet screw is shown in Figure 1-42:
Figure 1-42 Schematic diagram of the riveting process
Anchor rivet nut
Anchor riveting means that during the riveting process, part of the material of the riveted screw or nut is plastically deformed under the action of an external force, and a tight fit is formed with the base material, thereby realizing a reliable connection of the two parts.
The commonly used ZRS is connected to the substrate by this riveting type.
The riveting process is relatively simple, and the joint strength is low, and is usually used to limit the height of the fastener and to withstand a small torque. As shown in Figure 1-43:
Figure 1-43 Schematic diagram of the anchor riveting process
Pull rivet nut
The pull riveting means that the riveting member is plastically deformed under the action of external tension during the riveting process.
The position of the deformation is usually in a specially designed part, and the substrate is clamped by the deformation portion to achieve a reliable connection.
The commonly used rivet nuts are connected to the substrate by this riveting type.
The riveting is riveted using a special rivet gun, which is often used in places where the installation space is small and it is not possible to use universal riveting tools, such as closed pipes. As shown in Figure 1-44:
Figure 1-44 Schematic diagram of the pull riveting process
Floating rivet nut
Some of the rivet nuts on the sheet metal structure, because the overall chassis structure is complex, the accumulation error of the structure is too large, so that the relative position error of these rivet nuts is large, which makes assembly of other parts difficult.
This is a good improvement after the use of a riveted floating nut at the position of the corresponding rivet nut.
As shown in Figure 1-45: (Note: there must be enough space in the riveting position)
Figure 1-45 Schematic diagram of the press-fit process of the floating rivet nut
Anchor rivet nut or self-clinching rivet nut to the side distance
The anchor rivet nut or the self-clinching rivet nut are riveted together with the sheet by squeezing the sheet.
When the anchor riveting or self-clinching riveting is too close to the edge, it is easy to deform this part.
When there is no special requirement, the minimum distance between the center line of the riveted fastener and the edge of the sheet should be greater than L, see Figure 1-46.
Otherwise special clamps must be used to prevent the edges of the sheet from being deformed by force.
Figure 1-46 Minimum distance between the center line and the edge of the sheet
Factors affecting the quality of riveting
There are many factors affecting the quality of riveting. To sum up, there are mainly the following: substrate performance, bottom hole size, and riveting method.
1) Substrate properties.
When the hardness of the substrate is appropriate, the riveting quality is good, and the force of the riveting member is good.
2) Bottom hole size.
The size of the bottom hole directly affects the quality of the riveting, if the opening is large, then the gap between the substrate and the rivet is large.
For the riveting, there must not be enough deformation to fill the groove on the riveting piece, so that the shearing force is insufficient, which directly affects the thrust resistance of the riveting nut (nail).
For the rivet screw, the bottom hole is too large, and the pressing force generated by the plastic deformation during the riveting process becomes small, which directly affects the thrust resistance and the torsion resistance of the rivet screw (female).
The same for the riveting, the bottom hole is too large, so that the effective friction between the two pieces after plastic deformation is reduced, affecting the quality of the riveting.
The size of the bottom hole is small, although the force of the riveting can be increased to a certain extent, but the appearance quality of the riveting is likely to be poor.
The riveting force is large, the installation is inconvenient, and the deformation of the bottom plate is easily caused, which affects the production efficiency of the riveting work and the quality of the riveting.
3) Riveting method.
It has been introduced in the previous section. Riveting screws and nuts should pay great attention to the occasions in the process of use. Different situations and different force requirements require different types.
If it is not used properly, it will reduce the force range of the riveted screws and nuts, causing the connection to fail.
Here are a few examples to illustrate the correct use of the normal situation.
1) Do not install steel or stainless steel riveted fasteners before the aluminum plate is anodized or surface treated.
2) If there is too much riveting on the same straight line, there is no place for the extruded material to flow, which will generate a large stress and bend the workpiece into a curved shape.
3) Try to ensure that the surface of the board is plated before installing the riveted fasteners.
4) M5, M6, M8, M10 nuts are generally welded. Too large nuts generally require high strength. Arc welding can be used. Below M4 (including M4) the anchor rivet nut should be used. If it is electroplated, the rivet nut with electroless plating can be used.
5) When riveting the nut on the bent side, in order to ensure the riveting quality of the riveted nut, it is necessary to pay attention to: 1. The distance from the edge of the riveting hole to the side of the bend must be greater than the deformation zone of the bent part. 2. The distance L from the center of the riveted nut to the inside of the bent side should be greater than the sum of the outer cylindrical radius of the riveted nut and the inner radius of the bend. That is, L>D/2+r.
Projection weld nut
The projection weld nut (spot weld nut) is widely used in the design of sheet metal parts.
However, in many designs, the size of the pre-hole is not in accordance with the standard and cannot be accurately positioned.
The structural type and dimensions are as shown in Figure 1-47 and Figure 1-48. The recommended values for the hole diameter D0 and the thickness H before welding of the steel plate for welding are as specified in Table 1-17.
Figure 1-47 Welding hex nut structure type
Figure 1-48 Welding of welded hex nuts and steel plates
Table 1-17 Welded hex nut dimensions and opening thickness of corresponding steel plate (mm)
|Thread size (D or D×P)||M4||M5||M6||M8||M10||M12||M16|
|─||─||─||M8×1||M10×1||M12×1. 5||M16×1. 5|
Note: Do not use the specifications in parentheses as much as possible.
Hole flanging & tapping
Common coarse threaded boring size
|Thread diameter M||Thickness t||Inner diameter D1||Outer diameter D2||Height h||Pre-punch diameter D0||Radius|
The minimum distance from the tapping to the bending edge
Table 1-19 Distance between the tapping center and the bending edge H value comparison table
|Thickness / thread diameter||1||1.2||1.5||2|
Comparison of rivet nuts, self-clinching nut, riveting, and hole flanging & tapping
Table 1-20 Comparison of the rivet nut, self-clinching nut, pull riveting, and the tapping
|Connection method / feature||Anchor rivet nut||self-clinching rivet nut||pull riveting||flanging & tapping|
|Processability||it is good||good||good||average|
|Sheet metal requirements||Stainless steel riveting, easy to fall off||Stainless steel riveting is very poor, use special rivet nuts, and need spot welding||none||Thin plate and copper, aluminum soft material easy to slip|
|Durability||good||good||good||Copper and aluminum soft materials are poor, other material threads have 3 to 4 buckles or more|
1.5 Sheet Metal Drawing
Common stretch forms and design considerations
The sheet metal stretch is shown in Figure 1-50.
Figure 1-50 Sheet metal stretching design
Sheet metal stretch considerations:
- The minimum fillet radius between the bottom and the wall of the tensile member should be greater than the thickness of the plate, ie r1>t; in order to make the stretching smoother, generally take r1=(3~5)t, the maximum fillet radius It should be less than 8 times the thickness of the plate, ie r1 < 8t.
- The minimum fillet radius between the flange and the wall of the tensile member should be greater than 2 times the thickness of the plate, ie r2>2t; in order to make the stretching smoother, generally take r2=5t, the maximum fillet radius should be less than 8 times the thickness of the plate, ie r1 < 8t.
- The diameter of the inner cavity of the circular tensile partsshould be D≥d+12t, so that the pressure plate is not pressed when it is stretched.
- The minimum cornerradius between adjacent walls of the rectangular tensile partsshould be r3 ≥ 3t. In order to reduce the number of stretching, take r3 ≥ 1/5H as much as possible to complete the stretching.
- The tensile strength of thepartschanges after being stretched. Generally, the center of the bottom is kept at the original thickness, the material at the bottom corners is thinned, the material at the top near the flange is thickened, and the material at the rounded corners of the rectangular tensile parts becomes thick. When designing a stretched product, it is clearly stated on the drawing that the external dimensions or internal and external dimensions must be guaranteed, and the internal and external dimensions cannot be marked at the same time.
- The material thickness of the tensile member generally considers the rulethat the upper and lower wall thicknesses are not equal in the process deformation (ie, the upper thickness is thinner).
- When the circular flangeless tensile partsis formed at one time, the ratio of the height H to the diameter d should be less than or equal to 0.4.
Convex process size
In the shape and size of the convex sheet metal, several series sizes are specified in the sheet metal mold manual. There is a corresponding Form model in the Intralink library. The design should be selected according to the size specified in the manual, and the Form mold in the library is directly used.
Figure 1-51 Convex on sheet metal
Limit size of convex pitch and convex margin
Table 1-21 Limit dimensions of the convex pitch and the convex margin
Local depression and pressure line
As shown in 1-52, a 0.3-inch half-cut embossing on a sheet metal can be used as a sticker for a label or the like to improve the reliability of the label.
Such a semi-cutting concave, the deformation is much smaller than the normal stretching, but there is still a certain deformation for a large-area cover plate and a bottom plate which are not bent or have a small bending height.
Alternative method: Two right angle lines can be punched in the labeling range to improve the deformation. However, the reliability of the label attachment is reduced.
This method can also be used for processing such as product coding, production date, version, and even pattern.
Figure 1-52 Sinking and pressing line
Pressing the ribs on the plate-shaped metal parts, see Figure 1-53, helps to increase the structural rigidity.
Figure 1-53 Symmetrical structure of the rib
When marking the relevant dimensions of the curved part, consider the processability
Figure 1-54 Example of curved part labeling
As shown in Figure 1-54,
- a) After the punching and bending, the L dimension accuracy is easy to ensure and the processing is convenient.
- b) and c) If the accuracy of the dimension L is high, it is necessary to machine the hole after bending. The processing is very troublesome, and it is better not to use it.
1.6 Other Process Techniques
The drilling riveting is a riveting method between sheet metal, mainly used for the connection of coated steel plates or stainless steel plates.
One of the parts is punched, and the other part is punched and cuffed to make it a non-detachable connector.
Advantages: the flange is matched with the straight hole, and it has the positioning function itself. The riveting strength is high, and the riveting efficiency through the mold is also high. The specific way is as shown in Figure 1-55:
Figure 1-55 Drilling and riveting
Table 1-22 Drilling riveting dimensions
|Parameter||Thickness T(mm)||Flanging height H(mm)||Flanging outer dia. D(mm)|
|Corresponding straight hole inner dia. d and pre-punching hole d0|
Note: With the general principle H=T+T’+(0.3~0.4)
D = D’-0.3;
When T≧0.8mm, the wall thickness of the flanged hole is 0.4T.
When T<0.8mm, the wall thickness of the flange is usually 0.3mm. H is usually 0.46±0.12
In the sheet metal riveting method, there is also a riveting method that is the Tox riveting.
The principle is that two stacks are placed together, as shown in Figure 1-56.
Stamping and drawing using a mold, mainly used for the connection of coated steel sheets or stainless steel sheets.
It has the advantages of energy saving, environmental protection and high efficiency.
In the past, the chassis of the communication industry used more riveting, but the quality control of mass production was difficult. It has been applied less and is not recommended.
Figure 1-56 Tox riveting
1.7 Uniform Size of the Countersunk Head
Screw counterbore size
The structural dimensions of the screw counterbore are selected as shown in the following table.
For the countersunk head of the countersunk screw, if the plate is too thin, it is difficult to ensure the via d2 and the counterbore D at the same time, and the via d2 should be preferentially guaranteed.
Countersunk head and via for countersunk screws: (Selected sheet thickness t is preferably greater than h)
Table 1-23 Dimensions of screw counterbore
|Preferred min thickness||1.2||1.5||1.5||2||2|
Uniformity of the size of the counterbore of the countersunk head rivet
Table 1-24 Dimensions of Counterbore Holes for Hole Countersunk Rivets
Special treatment of thin-plates with countersunk head screws
The connection of sheet metal is completed by M3 countersunk screws.
If the thickness of the plated hole is 1 mm, it is problematic according to the conventional method.
However, in the actual design, a large number of such problems are encountered.
The rivet nut is used below, and the diameter of the counterbore is 6mm, which can effectively complete the connection, as shown in the figure.
This size is used in a large number of insert box.
It is important to note that this type of connection requires that the bottom nut is anchor rivet nuts.
The self-clinching rivet nut and the tapping tap cannot complete the tightening connection.
Figure 1-57 Countersunk head screw connection
In order to standardize such dimensions, the d/D should be as follows:
Table 1-25 Unification of thin plate counterbore